Simplified modelling of steel frame connections under cyclic loading
|
|
- Christian Nelson
- 5 years ago
- Views:
Transcription
1 Simplified modelling of steel frame connections under cyclic loading Saher El-Khoriby 1), *Mohammed A. Sakr 2), Tarek M. Khalifa 3) and Mohammed Eladly 4) 1), 2), 3), 4) Department of Structural Engineering, Faculty of Engineering, Tanta University, Tanta, Egypt 2) ABSTRACT The behaviour of steel frame connections has been experimentally and numerically studied in the literature under cyclic loading; however, most of the suggested numerical studies established complicated three-dimensional models. In this paper, firstly, simplified finite element models of steel beam-to-column endplate connections under cyclic loading were developed using three- and two-dimensional shell models. Element types and material constitutive model of cyclic plasticity were described. To simulate the actual behaviour of connection, the interactions between connection components (endplate, column flange and bolts) were accurately modelled. Both nonlinearities of material and geometry were considered. The two proposed finite element models were compared with previously proposed by another researcher three-dimensional solid model, then the three models were verified by typical quasi-static test results for an extended endplate connection, including both failure modes and hysteretic curves. They proved their capability for predicting the actual behaviour of steel connections. In terms of CPU time, the two-dimensional shell model is the most effective among the three models. 1. Introduction During some earthquakes in the last few years (e.g. Tokyo earthquake in 2011), many steel structures suffered from failure of the welded connections. The need for alternative connections encouraged scholars to carry out more studies in this area. Presently, the cyclic behaviour of steel frame connections has been investigated by many researchers. Numerous experimental works were performed. (Tsai 1990), (Sumner 2002), (Broderick 2002), (Guo 2006), (Shi 2007) and (Loureiro 2012) studied the cyclic behaviour of steel endplate connections under severe cyclic loading. On the other hand, (Yorgun 2001) tested a number of beam-to-column welded joints. 1) Professor 2) Associate professor 3) Lecturer 4) Master s Student
2 All of the mentioned experimental studies have conducted considerable works on the steel frame connections performance, however, because of difficulties and high cost of carrying out tests (especially in cases of wide parametric studies), the finite element (FE) modelling is openly used at present. Consequently, there is a pressing need for more accurate numerical modelling to undertake parametric analysis. There were some reports for the numerical simulation of steel frame connections. For example, (Pacurar 2006) used Ls-Dyna explicit nonlinear solver to model a beam to column steel endplate connection with prestressed bolts. An algorithm of finite element model was proposed by (Razavi 2007). (Shi 2008) developed a three-dimensional finite element model to simulate and analyse the mechanical behaviour of different types of beam-to-column endplate connections with pretensioned bolts based on ANSYS. (Eldemerdash 2012) presented three-dimensional finite element models to study the monotonic behaviour of large capacity eight-bolt extended un-stiffened wide endplate steel connections, using ANSYS. The ABAQUS finite-element package was used by (Wheeler 2000) to analyse bolted moment endplate connections joining square and rectangular hollow sections that are subjected to pure bending, using three-dimensional model. (Diacuteaz 2011) developed a three-dimensional ANSYS finite element model of steel beam to column bolted extended endplate connections for use to obtain their rotational behaviour. A finite element simulation is used by (Gerami 2011) to study and compare the cyclic behaviour of fourteen specimens of endplate and T-stub bolted connections by changing the horizontal and vertical arrangement of bolts. (Wang 2013) established a three-dimensional (3D) finite element model of ABAQUS to study the seismic behaviour of steel frame endplate connections subjected to cyclic loadings. Most of these aforesaid numerical investigations developed three-dimensional models. In terms of time and calculation cost, performing a wide parametric study of connections under cyclic loadings, using 3D model, isn t economic. Therefore, proposing simplified FE models taking into account proper contact relations and nonlinear behaviours, to accurately simulate steel frame connections and predict their hysteretic behaviour, is needful. The study in this paper aims to establish two simplified models (3D and 2D shell models) capable to simulate the actual cyclic behaviour of steel frame connections. The details of the suggested models (Element types, material cyclic constitutive models and interactions between connections components) were described. The results of the suggested numerical models were compared with experimental data in order to validate their accuracy. 2. Finite Element Analysis 3. The FE simulation software ABAQUS (Analysis user's manual 2012) was used to establish three models, including 3D solid model, 3D shell model and 2D shell model, able to model the behaviour of steel frame connections accurately. Steel beam, column, endplate, rib stiffeners of endplate, column stiffeners and high strength bolts are the components of endplate connection. A 3D solid FE model of an extended endplate connection is shown in Fig. 1(a), while the interactions between the connection components are illustrated in Fig. Fig. 2.
3 Based on (Wang 2013) s numerical work, a 3D solid model was established, while the two other models were proposed in this paper. All parts of the two proposed models are presented in details as follows. (b) 3D shell model (a) 3D solid model (c) 2D shell model Fig. 1 Different FE models of an extended endplate connection. Fig. 2 Interactions between connection components (Wang 2013). 2.1 Element types, meshes and contact modelling D model using shell element A 4-node doubly curved thin or thick shell, reduced integration, hourglass control, finite membrane strains element (S4R) was adopted for H-shaped steel beams and columns. In the 3D shell model, to represent the actual behaviour of bolts, rigid plastic CARTESIAN elements from the ABAQUS library (Analysis user's manual 2012) were used, as connector elements between the nodes of endplate and column flange, as shown in Fig. 1(b). Connector behaviours can be defined in any connector with available components of
4 relative motion. Available components of relative motion are displacements and rotations that are not kinematically constrained. Multiple connector behaviours can be defined in the connector section (Analysis user's manual 2012). To model a Cartesian connector that represents a high-strength bolt, various connector behaviours were defined. Plasticity and elasticity behaviours were defined in the bolt axial force direction. In the other two directions, the bolt shear force directions, the defined behaviours were plasticity, elasticity and stop. There is also a contact between the surfaces of endplate and column flange. Contact properties of contact surfaces comprise two parts: tangent interaction and normal interaction. Hard contact was used for normal interaction. It signifies that no penetration is allowed and no tensile forces will be transmitted. Furthermore, there is no limit to the magnitude of contact pressure that can be transmitted when the surfaces are in contact. For the tangent interaction, the Coulomb friction has been used, which allows some relative motion of the surfaces (an elastic slip when they should be sticking. hile the surfaces are sticking (i.e. crit, where is the calculated shear stress and crit is the maximum transmitted shear stress, the magnitude of sliding is limited to this elastic slip (Analysis user's manual 2012). The friction coefficients are selected according to test results D model using plane stress shell element A 4-node bilinear plane stress quadrilateral element (CPS4) was adopted for H- shaped steel beams and columns. Rigid plastic CARTESIAN elements, as well as interaction between column flange and endplate, were defined as described in 3D shell model. Fig. 1(c) shows a 2D shell FE model of an extended endplate connection. 2.2 Material modelling When steel elements are subjected to cyclic loadings, a steel cyclic constitutive model is needed, which is different from the monotonic model. Presently, steel stress strain relationship is ordinarily defined as multi-linear forms. Those models, however, cannot give satisfying results under cyclic loading (Shi 2011). Based on (Wang 2013) s numerical modelling of steel connections, it is possible to conclude that the results calculated from the cyclic model were in better agreement with experiments for both loading and reloading processes. The cyclic model well predicted the hysteretic behaviour (Wang 2013). Regarding the cyclic tests of steel which were performed by (Shi 2011), the used hardening for steel is a combined one, consisting of both isotropic hardening and kinematic hardening. Based on plastoelasticity, (Chaboche 1986,1989) proposed a cyclic combined model. In ABAQUS, this model can be implemented as a plastic constitutive model, containing a nonlinear isotropic hardening component and a kinematic hardening component (Analysis user's manual 2012). 4. Verification of numerical analysis
5 In order to verify the capability of the suggested finite element models (3D and 2D shell models) to model steel beam-to-column bolted connections accurately, the typical quasi-static cyclic tests of steel endplate connections, which performed by (Shi 2007), was selected. 3.1 Tests of Shi et al. (Shi 2007) tested a series of eight full-scale structural steel beam-to-column endplate moment connection specimens under cyclic loads. The parameters investigated were endplate thickness, bolt diameter, endplate extended stiffener, column stiffener, type of flush and extended endplate. A typical extended endplate connection used for tests is shown in (a) Test specimen and loading arrangement (b) JD2 details Fig. 3(a). The out-of-plane deformations of the specimens were restrained during tests. These eight specimens are all beam-to-column connections that originated from typical multi-storey steel frames. Specimen (JD2) was selected to be modelled using the three previously mentioned models (three-dimensional solid model established by (Wang 2013) and three- and two-dimensional shell models) to verify their accuracy. The details of JD2 specimen are shown in
6 (a) Test specimen and loading arrangement Fig. 3(b). (b) JD2 details (a) Test specimen and loading arrangement (b) JD2 details Fig. 3 Test specimen, loading arrangement and connection details (Shi 2007). The depth, web thickness and flange thickness of columns and beams are 300 mm, 8 mm and 12 mm, and the column and beam width are 250 mm and 200 mm respectively. The thickness of the column flange is the same as the endplate within the range of 100 mm above and below the extension edge of the endplate. The thickness of the column stiffener and endplate extended stiffener is 12 mm and 10 mm respectively. The specimens tested in Shi el al. tests were fabricated from Q345B steel. According to (Shi 2011) s models, the parameters of steel under cyclic loading are shown in
7 Table 1. Pre-tension force of bolts was imposed first with a value of 199 kn for specimen (JD2). The grade of the bolts was According to (Shi 2008 s numerical simulation results, the coefficient of friction between steel surfaces was considered as The cyclic loading procedure was a load/displacement control method. σ 0 Q Table 1 Calibration parameters of steel (Wang 2013). b C 1 ɣ 1 C 2 ɣ 2 C 3 ɣ 3 C Comparison of tests and numerical analysis From Fig. 4, the three finite element models accurately simulated the hysteretic behaviour of the extended endplate connection. It was observed that slight pinching phenomenon of hysteretic curve has occurred after the unloading process. From comparative curves, the three numerical methods simulated this phenomenon well. ɣ 4 Fig. 4 Comparison of measured and predicted moment rotation hysteretic curves for extended endplate connection. The carrying capacity of the JD2 specimen was predicted. Comparison of experimental and numerical results is shown in The errors in predicting the maximum capacity were less than 2% for the three models. Table 2. The errors in predicting the maximum capacity were less than 2% for the three models.
8 3] Table 2 Ultimate moment comparison of the three FE models and test results. Test 3D solid model (Wang 2013) 3D Shell model 2D Shell model M max (kn.m) Comparison of the three models CPU time Table 3 illustrates a comparison of the CPU time of the three models for an endplate frame connection. It shows a great difference in the CPU time between the three models. To model an extended endplate connection under cyclic loading, the 2D shell model consumed about 25% of the 3D shell model CPU time and about 2.3% of the 3D solid model CPU time, which indicated that the 2D shell model is the most effective among the three models. Table 3 CPU time comparison of the three FE models. 3D solid model 3D Shell model 2D Shell model CPU Time (minutes) Conclusions Three models (3D solid, 3D shell and 2D shell models) were established to simulate the cyclic behaviour of steel frame connections. Based on previous numerical work, the 3D solid model was established, while the two other models were proposed in this paper. The two proposed models were verified by the results of steel frame connections typical quasi-static tests. The proposed 3D and 2D shell models evidenced their capability to predict accurately the cyclic behaviour of steel bolted connections, but the 2D shell model was the most effective among the three studied models. It consumed about 25% of the 3D shell model CPU time and almost 2.3% of the 3D solid model CPU time. This simplified model provided a strong tool for studying the connections behaviours. References [ 1 [2ABAQUS. Analysis user's manual. (2012), Version USA: ABAQUS, Inc., Dassault Systèmes. Broderick, B.M. and Thomson, A.W. (2002, The response of flush endplate joints under earthquake loading, J Constr Steel Res, 58(9), [[4]Chaboche, J.L. (1986, Time independent constitutive theories for cyclic plasticity, Int J Plast, 2(2), [5]Chaboche, J.L. (1989), Constitutive equations for cyclic plasticity and cyclic viscoplasticity, Int J Plast, 5(3), Diacuteaz, C., Victoria, M. and Martiacute, P. (2011, FE model of beam-to-column extended endplate joints, J Constr Steel Res, 67(10),
9 [ [12] [13] [6]Eldemerdash, M., Abu-Lebdeh, T. and Al Nasra M. (2012, Finite element analysis of large capacity endplate steel connections, J Comput Sci, 8(4), ]Gerami, M., Saberi, H. and Saberi V. (2011), Cyclic behavior of bolted connections with different arrangement of bolts, J Constr Steel Res, 67(4), Guo, B., Gu, Q. and Liu, F. (2006, Experimental behavior of stiffened and un-stiffened endplate connections under cyclic loading, J Struct Eng, ASCE, 132(9), Loureiro, A., Moreno, A. and Gutierrez, R. (2012, Experimental and numerical analysis of three-dimensional semi-rigid steel joints under non-proportional loading, Eng Struct, 38, Pacurar, V., Petrina, M. and Lupea, I. (2006, Numerical analysis of the behavior of semi rigid beam to column connections of steel frames, International Conference on Metal Structures, Poiana Brasov, ROMANIA. Razavi, H., Abolmaali, A. and Ghassemieh, M. (2007, Invisible elastic bolt model concept for finite element analysis of bolted connections, J Constr Steel Res, 63(5), [9]Shi, G., Shi, Y.J. and Wang, Y.Q. (2007, Behaviour of endplate moment connections under earthquake loading, Eng Struct, 29(5), ]Shi, G., Shi, Y.J. and Wang, Y.Q. (2008, Numerical simulation of steel pre-tensioned bolted endplate connections of different types and details, Eng Struct, 30(10), [11]Shi, Y.J., Wang, M. and Wang, Y.Q. (2011, Experimental and constitutive model study of structural steel under cyclic loading, J Constr Steel Res, 67(8), Sumner, E.A. and Murray, T.M. (2002, Behavior of extended endplate moment connections subject to cyclic loading, J Struct Eng, ASCE, 128(4), Tsai, K.C. and Popov, E.P. (1990, Cyclic behavior of end-plate moment connections, J Struct Eng, ASCE, 116(11), [14]Wang, M., Shi, Y.J., Wang, Y.Q. and Shi, G. (2013, Numerical study on seismic behaviors of steel frame endplate connections, J Constr Steel Res, 90, ]Wheeler, A.T., Clarke, M.J. and Hancock G.J. (2000, FE modeling of four-bolt, tubular moment endplate connections, J Struct Eng, ASCE, 126(7), Yorgun, C. and Bayramoglu, G. (2001, Cyclic tests for welded-plate sections with endplate connections, J Constr Steel Res, 57(12),
Non-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla
Non-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla 1 Faculty of Civil Engineering, Universiti Teknologi Malaysia, Malaysia redzuan@utm.my Keywords:
More informationstudying of the prying action effect in steel connection
studying of the prying action effect in steel connection Saeed Faraji Graduate Student, Department of Civil Engineering, Islamic Azad University, Ahar Branch S-faraji@iau-ahar.ac.ir Paper Reference Number:
More informationStrength of Overlapping Multi-Planar KK Joints in CHS Sections
Strength of Overlapping Multi-Planar KK Joints in CHS Sections Peter Gerges 1, Mohamed Hussein 1, Sameh Gaawan 2 Structural Engineer, Department of Structures, Dar Al-Handasah Consultants, Giza, Egypt
More informationAvailable online at ScienceDirect. Procedia Engineering 160 (2016 )
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 16 (216 ) 11 18 XVIII International Colloquium on Mechanical Fatigue of Metals (ICMFM XVIII) Characterization of the cyclic
More informationThrough Process Modelling of Self-Piercing Riveting
8 th International LS-DYNA User Conference Metal Forming (2) Through Process Modelling of Self-Piercing Riveting Porcaro, R. 1, Hanssen, A.G. 1,2, Langseth, M. 1, Aalberg, A. 1 1 Structural Impact Laboratory
More informationWP1 NUMERICAL BENCHMARK INVESTIGATION
WP1 NUMERICAL BENCHMARK INVESTIGATION 1 Table of contents 1 Introduction... 3 2 1 st example: beam under pure bending... 3 2.1 Definition of load application and boundary conditions... 4 2.2 Definition
More informationAdvanced model of steel joints loaded by internal forces from 3D frame structures
Advanced model of steel joints loaded by internal forces from 3D frame structures Lubomír Šabatka, IDEA RS s.r.o František Wald, FSv ČVUT Praha Jaromír Kabeláč, Hypatia Solutions s.r.o Drahoslav Kolaja,
More informationSome Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact
Some Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact Eduardo Luís Gaertner Marcos Giovani Dropa de Bortoli EMBRACO S.A. Abstract A linear elastic model is often not appropriate
More informationCHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING
113 CHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING 6.1 INTRODUCTION Superplastic properties are exhibited only under a narrow range of strain rates. Hence, it
More informationA Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections
A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections Dawit Hailu +, Adil Zekaria ++, Samuel Kinde +++ ABSTRACT After the 1994 Northridge earthquake
More informationEngineering Solid Mechanics
Engineering Solid Mechanics 2 (2013) 51-66 Contents lists available at GrowingScience Engineering Solid Mechanics homepage: www.growingscience.com/esm Modeling and FE analysis of column to beam end-plate
More informationCHAPTER-10 DYNAMIC SIMULATION USING LS-DYNA
DYNAMIC SIMULATION USING LS-DYNA CHAPTER-10 10.1 Introduction In the past few decades, the Finite Element Method (FEM) has been developed into a key indispensable technology in the modeling and simulation
More informationThe Open Civil Engineering Journal
Send Orders for Reprints to reprints@benthamscience.ae 250 The Open Civil Engineering Journal Content list available at: www.benthamopen.com/tociej/ DOI: 10.2174/1874149501812010250, 2018, 12, 250-262
More information1.2 Connection configurations:
1.2 Connection configurations: 1.2.1 Simple connections: Simple connections are assumed to transfer shear only shear at some nominal eccentricity. Therefore such connections can be used only in non-sway
More informationModelling Flat Spring Performance Using FEA
Modelling Flat Spring Performance Using FEA Blessing O Fatola, Patrick Keogh and Ben Hicks Department of Mechanical Engineering, University of Corresponding author bf223@bath.ac.uk Abstract. This paper
More informationFinite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint
Finite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint Jose M. Cabrero Assistant Professor University of Navarra, Department of Structural Analysis and Design,
More informationOptimal Stiffeners Spacing for Intermediate Link in Eccentrically Braced Frame to Increase Energy Dissipation
AUT Journal of Civil Engineering AUT J. Civil Eng., 1(1) (2017) 39-44 DOI: 10.22060/ceej.2017.12345.5176 Optimal Stiffeners Spacing for Intermediate Link in Eccentrically Braced Frame to Increase Energy
More informationCHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force
CHAPTER 4 Numerical Models This chapter presents the development of numerical models for sandwich beams/plates subjected to four-point bending and the hydromat test system. Detailed descriptions of the
More informationOPTIMIZATION OF ENERGY DISSIPATION PROPERTY OF ECCENTRICALLY BRACED STEEL FRAMES
OPTIMIZATION OF ENERGY DISSIPATION PROPERTY OF ECCENTRICALLY BRACED STEEL FRAMES M. Ohsaki (Hiroshima Univ.) T. Nakajima (Kyoto Univ. (currently Ohbayashi Corp.)) Background Difficulty in optimization
More informationFinite Element Buckling Analysis Of Stiffened Plates
International Journal of Engineering Research and Development e-issn: 2278-067X, p-issn: 2278-800X, www.ijerd.com Volume 10, Issue 2 (February 2014), PP.79-83 Finite Element Buckling Analysis Of Stiffened
More informationCHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS
CHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS 7.1 GENERAL An analytical study on behaviour of combined effect of optimised channel sections using ANSYS was carried out and discussed in
More informationSettlement Analysis of Piled Raft Foundation System (PRFS) in Soft Clay
IOSR Journal of Mechanical and Civil Engineering (IOSR-JMCE) e-issn: 2278-1684,p-ISSN: 2320-334X, Volume 14, Issue 2 Ver. VIII (Mar. - Apr. 2017), PP 62-68 www.iosrjournals.org Settlement Analysis of Piled
More informationConfiguration Optimization of Anchoring Devices of Frame-Supported Membrane Structures for Maximum Clamping Force
6 th China Japan Korea Joint Symposium on Optimization of Structural and Mechanical Systems June 22-25, 200, Kyoto, Japan Configuration Optimization of Anchoring Devices of Frame-Supported Membrane Structures
More informationAnalyzing Elastomer Automotive Body Seals Using LS-DYNA
7 th International LS-DYNA Users Conference Methods Development Analyzing Elastomer Automotive Body Seals Using LS-DYNA Linhuo Shi TG North America Corporation 95 Crooks Road Troy, MI 4884 Tel: (248) 28-7348
More informationModeling Foundations in RS
Modeling Foundations in RS 3 Piled Raft Modeling in RS 3 Deep foundation piles are commonly used to increase foundation stability and to increase the bearing capacity of structural systems. The design
More informationScientific Manual FEM-Design 17.0
Scientific Manual FEM-Design 17. 1.4.6 Calculations considering diaphragms All of the available calculation in FEM-Design can be performed with diaphragms or without diaphragms if the diaphragms were defined
More informationCase Study - Vierendeel Frame Part of Chapter 12 from: MacLeod I A (2005) Modern Structural Analysis, ICE Publishing
Case Study - Vierendeel Frame Part of Chapter 1 from: MacLeod I A (005) Modern Structural Analysis, ICE Publishing Iain A MacLeod Contents Contents... 1 1.1 Vierendeel frame... 1 1.1.1 General... 1 1.1.
More informationOrbital forming of SKF's hub bearing units
Orbital forming of SKF's hub bearing units Edin Omerspahic 1, Johan Facht 1, Anders Bernhardsson 2 1 Manufacturing Development Centre, AB SKF 2 DYNAmore Nordic 1 Background Orbital forming is an incremental
More informationNon-Linear Analysis of Base Plates in Automated Storage Systems
Non-Linear Analysis of Base Plates in Automated Storage Systems Ph.D. Juan José del Coz Díaz, Fco. Suarez Domínguez, Paulino J.Garcia Nieto University of Oviedo. Construction and Applied Mathematics Area.
More informationTHREE DIMENSIONAL ACES MODELS FOR BRIDGES
THREE DIMENSIONAL ACES MODELS FOR BRIDGES Noel Wenham, Design Engineer, Wyche Consulting Joe Wyche, Director, Wyche Consulting SYNOPSIS Plane grillage models are widely used for the design of bridges,
More informationIntroduction to Abaqus. About this Course
Introduction to Abaqus R 6.12 About this Course Course objectives Upon completion of this course you will be able to: Use Abaqus/CAE to create complete finite element models. Use Abaqus/CAE to submit and
More informationTABLE OF CONTENTS SECTION 2 BACKGROUND AND LITERATURE REVIEW... 3 SECTION 3 WAVE REFLECTION AND TRANSMISSION IN RODS Introduction...
TABLE OF CONTENTS SECTION 1 INTRODUCTION... 1 1.1 Introduction... 1 1.2 Objectives... 1 1.3 Report organization... 2 SECTION 2 BACKGROUND AND LITERATURE REVIEW... 3 2.1 Introduction... 3 2.2 Wave propagation
More informationA Computational Study of Local Stress Intensity Factor Solutions for Kinked Cracks Near Spot Welds in Lap- Shear Specimens
A Computational Study of Local Stress ntensity Factor Solutions for Kinked Cracks Near Spot Welds in Lap- Shear Specimens D.-A. Wang a and J. Pan b* a Mechanical & Automation Engineering, Da-Yeh University,
More informationExample 24 Spring-back
Example 24 Spring-back Summary The spring-back simulation of sheet metal bent into a hat-shape is studied. The problem is one of the famous tests from the Numisheet 93. As spring-back is generally a quasi-static
More informationEVALUATION OF THE COMPLETE MOMENT-ROTATION CURVE of bolted beam-to-column connections using mechanical models
EUROSTEEL 28, 3-5 September 28, Graz, Austria 579 EVALUATION OF THE COMPLETE MOMENT-ROTATION CURVE of bolted beam-to-column connections using mechanical models Minas Lemonis and Charis Gantes National
More informationBehaviour of cold bent glass plates during the shaping process
Behaviour of cold bent glass plates during the shaping process Kyriaki G. DATSIOU *, Mauro OVEREND a * Department of Engineering, University of Cambridge Trumpington Street, Cambridge, CB2 1PZ, UK kd365@cam.ac.uk
More informationNumerical Modelling of Cross Roll Straightening
7. LS-DYNA Anwenderforum, Bamberg 2008 Metallumformung I Numerical Modelling of Cross Roll Straightening A. Mutrux, B. Berisha, B. Hochholdinger, P. Hora Institute of Virtual Manufacturing, ETH Zurich
More informationCollapse Analyses on Spirally Welded Tapered Tubes using EC3 Generated Imperfections
Proceedings of the Annual Stability Conference Structural Stability Research Council Orlando, Florida, April 12-15, 2016 Collapse Analyses on Spirally Welded Tapered Tubes using EC3 Generated Imperfections
More informationChapter 3 Analysis of Original Steel Post
Chapter 3. Analysis of original steel post 35 Chapter 3 Analysis of Original Steel Post This type of post is a real functioning structure. It is in service throughout the rail network of Spain as part
More informationParametric Study of Beam to Column Bolted Connection with Cellular Beams
Parametric Study of Beam to Column Bolted Connection with Cellular Beams Anju Mohan 1, Dr. K. A Abubaker 2, Lakshmi G Das 3 1Department of Civil Engineering, IIET, Nellikuzhy 2Chief Consultant, SAFE, Edappally
More informationTechnical Report Example (1) Chartered (CEng) Membership
Technical Report Example (1) Chartered (CEng) Membership A TECHNICAL REPORT IN SUPPORT OF APPLICATION FOR CHARTERED MEMBERSHIP OF IGEM DESIGN OF 600 (103 BAR) 820MM SELF SEALING REPAIR CLAMP AND VERIFICATION
More informationES 128: Computer Assignment #4. Due in class on Monday, 12 April 2010
ES 128: Computer Assignment #4 Due in class on Monday, 12 April 2010 Task 1. Study an elastic-plastic indentation problem. This problem combines plasticity with contact mechanics and has many rich aspects.
More informationStep Change in Design: Exploring Sixty Stent Design Variations Overnight
Step Change in Design: Exploring Sixty Stent Design Variations Overnight Frank Harewood, Ronan Thornton Medtronic Ireland (Galway) Parkmore Business Park West, Ballybrit, Galway, Ireland frank.harewood@medtronic.com
More informationRecent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA
14 th International LS-DYNA Users Conference Session: Simulation Recent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA Hailong Teng Livermore Software Technology Corp. Abstract This paper
More informationDESIGN AND ANALYSIS OF MEMBRANE STRUCTURES IN FEM-BASED SOFTWARE MASTER THESIS
DESIGN AND ANALYSIS OF MEMBRANE STRUCTURES IN FEM-BASED SOFTWARE MASTER THESIS ARCHINEER INSTITUTES FOR MEMBRANE AND SHELL TECHNOLOGIES, BUILDING AND REAL ESTATE e.v. ANHALT UNIVERSITY OF APPLIED SCIENCES
More informationFINITE ELEMENT ANALYSIS OF A COMPOSITE CATAMARAN
NAFEMS WORLD CONGRESS 2013, SALZBURG, AUSTRIA FINITE ELEMENT ANALYSIS OF A COMPOSITE CATAMARAN Dr. C. Lequesne, Dr. M. Bruyneel (LMS Samtech, Belgium); Ir. R. Van Vlodorp (Aerofleet, Belgium). Dr. C. Lequesne,
More informationOptimization of Energy Dissipation Property of Eccentrically Braced Steel Frames
9 th World Congress on Structural and Multidisciplinary Optimization June 13-17, 2010, Shizuoka, Japan Optimization of Energy Dissipation Property of Eccentrically Braced Steel Frames Makoto Ohsaki 1,
More informationINTERNATIONAL DISTRIBUTED HYBRID SIMULATION OF 2-SPAN CONTINUOUS BRIDGE
INTERNATIONAL DISTRIBUTED HYBRID SIMULATION OF 2-SPAN CONTINUOUS BRIDGE Y. Takahashi 1, H. Iemura 2, S.A. Mahin 3 and G.L. Fenves 4 1 Associate Professor, Disaster Prevention Research Institute, Kyoto
More informationStrain-Based Finite Element Analysis of Stiffened Cylindrical Shell Roof
American Journal of Civil Engineering 2017; 5(4): 225-230 http://www.sciencepublishinggroup.com/j/ajce doi: 10.11648/j.ajce.20170504.15 ISSN: 2330-8729 (Print); ISSN: 2330-8737 (Online) Strain-Based Finite
More informationRevision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction
Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to
More informationDifficulties in FE-modelling of an I- beam subjected to torsion, shear and bending
DEGREE PROJECT, IN STEEL STRUCTURES, SECOND LEVEL STOCKHOLM, SWEDEN 2015 Difficulties in FE-modelling of an I- beam subjected to torsion, shear and bending MIRIAM ALEXANDROU KTH ROYAL INSTITUTE OF TECHNOLOGY
More informationThe Open Construction and Building Technology Journal
Send Orders for Reprints to reprints@benthamscience.ae The Open Construction and Building Technology Journal, 2018, 12, (Suppl-1, M11) 177-186 177 The Open Construction and Building Technology Journal
More informationGuidelines for proper use of Plate elements
Guidelines for proper use of Plate elements In structural analysis using finite element method, the analysis model is created by dividing the entire structure into finite elements. This procedure is known
More informationVIRTUAL TESTING OF AIRCRAFT FUSELAGE STIFFENED PANELS
4 TH INTERNATIONAL CONGRESS OF THE AERONAUTICAL SCIENCES VIRTUAL TESTING OF AIRCRAFT FUSELAGE STIFFENED PANELS Peter Linde*, Jürgen Pleitner*, Wilhelm Rust** *Airbus, Hamburg, Germany, **CAD-FE GmbH, Burgdorf
More informationPrint Depth Prediction in Hot Forming Process with a Reconfigurable Die
Print Depth Prediction in Hot Forming Process with a Reconfigurable Die Jonathan Boisvert* Thibaut Bellizzi* Henri Champliaud Patrice Seers École de Technologie supérieure, Montréal, Québec *Master students,
More informationInvestigation of seat modelling for sled analysis and seat comfort analysis with J-SEATdesigner
Investigation of seat modelling for sled analysis and seat comfort analysis with J-SEATdesigner Noriyo ICHINOSE 1, Hideki YAGI 1 1 JSOL Corporation, Nagoya, Japan 1 Abstract Recently vehicle model is becoming
More information3D Finite Element Software for Cracks. Version 3.2. Benchmarks and Validation
3D Finite Element Software for Cracks Version 3.2 Benchmarks and Validation October 217 1965 57 th Court North, Suite 1 Boulder, CO 831 Main: (33) 415-1475 www.questintegrity.com http://www.questintegrity.com/software-products/feacrack
More informationModel Set up, Analysis and Results of the Inverse Forming Tool in ANSA
Model Set up, Analysis and Results of the Inverse Forming Tool in ANSA Evlalia Iordanidou, Georgios Mokios BETA CAE Systems SA Abstract With an ongoing aim to reduce the time a model requires to be prepared,
More informationThe Finite Element Method for the Analysis of Non-Linear and Dynamic Systems. Prof. Dr. Eleni Chatzi, J.P. Escallo n Lecture December, 2013
The Finite Element Method for the Analysis of Non-Linear and Dynamic Systems Prof. Dr. Eleni Chatzi, J.P. Escallo n Lecture 11-17 December, 2013 Institute of Structural Engineering Method of Finite Elements
More informationLateral Loading of Suction Pile in 3D
Lateral Loading of Suction Pile in 3D Buoy Chain Sea Bed Suction Pile Integrated Solver Optimized for the next generation 64-bit platform Finite Element Solutions for Geotechnical Engineering 00 Overview
More informationVehicle Load Area Division Wall Integrity during Frontal Crash
Vehicle Load Area Division Wall Integrity during Frontal Crash H. Türkmen TOFAS Türk Otomobil Fabrikasi A.S. Abstract : This study addresses design efforts of a vehicle load area division wall and the
More informationSimplified Design Procedure for Piles Affected by Lateral Spreading based on 3D Nonlinear FEA Using OpenSees. University of Washington
Simplified Design Procedure for Piles Affected by Lateral Spreading based on 3D Nonlinear FEA Using OpenSees Christopher R. McGann, Ph.D. Student Pedro Arduino Peter Mackenzie-Helnwein University of Washington
More informationPLAXIS 2D - SUBMERGED CONSTRUCTION OF AN EXCAVATION
PLAXIS 2D - SUBMERGED CONSTRUCTION OF AN EXCAVATION 3 SUBMERGED CONSTRUCTION OF AN EXCAVATION This tutorial illustrates the use of PLAXIS for the analysis of submerged construction of an excavation. Most
More informationSolid and shell elements
Solid and shell elements Theodore Sussman, Ph.D. ADINA R&D, Inc, 2016 1 Overview 2D and 3D solid elements Types of elements Effects of element distortions Incompatible modes elements u/p elements for incompressible
More informationApplication of Predictive Engineering Tool (ABAQUS) to Determine Optimize Rubber Door Harness Grommet Design
Application of Predictive Engineering Tool (ABAQUS) to Determine Optimize Rubber Door Harness Grommet Design Praveen Mishra, Dayananda Gowda Mercedes Benz R & D India, Bangalore, Karnataka, India Abstract:
More informationModule 1: Introduction to Finite Element Analysis. Lecture 4: Steps in Finite Element Analysis
25 Module 1: Introduction to Finite Element Analysis Lecture 4: Steps in Finite Element Analysis 1.4.1 Loading Conditions There are multiple loading conditions which may be applied to a system. The load
More informationCrashbox Tutorial. In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0
Crashbox Tutorial In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0 (Written by Moritz Guenther, student at Altair Engineering GmbH) 1 HyperMesh* 1. Start
More informationFREE VIBRATION AND EARTHQUAKE ANALYSIS OF A BUILDING
14 FREE VIBRATION AND EARTHQUAKE ANALYSIS OF A BUILDING This example demonstrates the natural frequency of a five-storey building when subjected to free vibration and earthquake loading. The building consists
More informationFigure 30. Degrees of freedom of flat shell elements
Shell finite elements There are three types of shell finite element; 1) flat elements, 2) elements based on the Sanders-Koiter equations and 3) elements based on reduction of a solid element. Flat elements
More informationEngineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering
Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Here SolidWorks stress simulation tutorials will be re-visited to show how they
More informationSet No. 1 IV B.Tech. I Semester Regular Examinations, November 2010 FINITE ELEMENT METHODS (Mechanical Engineering) Time: 3 Hours Max Marks: 80 Answer any FIVE Questions All Questions carry equal marks
More informationA MODELING METHOD OF CURING DEFORMATION FOR CFRP COMPOSITE STIFFENED PANEL WANG Yang 1, GAO Jubin 1 BO Ma 1 LIU Chuanjun 1
21 st International Conference on Composite Materials Xi an, 20-25 th August 2017 A MODELING METHOD OF CURING DEFORMATION FOR CFRP COMPOSITE STIFFENED PANEL WANG Yang 1, GAO Jubin 1 BO Ma 1 LIU Chuanjun
More informationRevised Sheet Metal Simulation, J.E. Akin, Rice University
Revised Sheet Metal Simulation, J.E. Akin, Rice University A SolidWorks simulation tutorial is just intended to illustrate where to find various icons that you would need in a real engineering analysis.
More informationGlobal to Local Model Interface for Deepwater Top Tension Risers
Global to Local Model Interface for Deepwater Top Tension Risers Mateusz Podskarbi Karan Kakar 2H Offshore Inc, Houston, TX Abstract The water depths from which oil and gas are being produced are reaching
More informationQuarter Symmetry Tank Stress (Draft 4 Oct 24 06)
Quarter Symmetry Tank Stress (Draft 4 Oct 24 06) Introduction You need to carry out the stress analysis of an outdoor water tank. Since it has quarter symmetry you start by building only one-fourth of
More informationWhat makes Bolt Self-loosening Predictable?
What makes Bolt Self-loosening Predictable? Abstract Dr.-Ing. R. Helfrich, Dr.-Ing. M. Klein (INTES GmbH, Germany) In mechanical engineering, bolts are frequently used as standard fastening elements, which
More informationEvaluation of LS-DYNA Material Models for the Analysis of Sidewall Curl in Advanced High Strength Steels
12 th International LS-DYNA Users Conference Constitutive Modeling(4) Evaluation of LS-DYNA Material Models for the Analysis of Sidewall Curl in Advanced High Strength Steels Ali Aryanpour *, Daniel E.
More informationElement Order: Element order refers to the interpolation of an element s nodal results to the interior of the element. This determines how results can
TIPS www.ansys.belcan.com 鲁班人 (http://www.lubanren.com/weblog/) Picking an Element Type For Structural Analysis: by Paul Dufour Picking an element type from the large library of elements in ANSYS can be
More informationSimulation of AJWSP10033_FOLDED _ST_FR
Phone: 01922 453038 www.hyperon-simulation-and-cad-services.co.uk Simulation of AJWSP10033_FOLDED _ST_FR Date: 06 May 2017 Designer: Study name: AJWSP10033_FOLDED_STATIC Analysis type: Static Description
More informationSimulation of Overhead Crane Wire Ropes Utilizing LS-DYNA
Simulation of Overhead Crane Wire Ropes Utilizing LS-DYNA Andrew Smyth, P.E. LPI, Inc., New York, NY, USA Abstract Overhead crane wire ropes utilized within manufacturing plants are subject to extensive
More informationTypes of Idealizations. Idealizations. Cylindrical Shaped Part. Cyclic Symmetry. 3D Shell Model. Axisymmetric
Types of Idealizations Idealizations Selecting the model type 3D Solid Plane Stress Plane Strain 3D Shell Beam Cyclic Symmetry Cylindrical Shaped Part Interior Pressure Load 3D model can be used to model
More informationMODELLING OF AN AUTOMOBILE TYRE USING LS-DYNA3D
MODELLING OF AN AUTOMOBILE TYRE USING LS-DYNA3D W. Hall, R. P. Jones, and J. T. Mottram School of Engineering, University of Warwick, Coventry, CV4 7AL, UK ABSTRACT: This paper describes a finite element
More informationFinite element modelling techniques and testing methods of submerged pipes
Visit the SIMULIA Resource Center for more customer examples. Finite element modelling techniques and testing methods of submerged pipes A. Giordano 1, A.C. Walker 2 and F. Guarracino 1 1 Dipartimento
More informationA Sensitivity Analysis On The Springback Behavior Of The Unconstrained Bending Problem
A Sensitivity Analysis On The Springback Behavior Of The Unconstrained Bending Problem T. Meinders 1,2, A.W.A. Konter 1, S.E. Meijers 1, E.H. Atzema 3, H. Kappert 4 1 Netherlands Institute for Metals Research,
More informationMAE 323: Lab 7. Instructions. Pressure Vessel Alex Grishin MAE 323 Lab Instructions 1
Instructions MAE 323 Lab Instructions 1 Problem Definition Determine how different element types perform for modeling a cylindrical pressure vessel over a wide range of r/t ratios, and how the hoop stress
More informationSUBMERGED CONSTRUCTION OF AN EXCAVATION
2 SUBMERGED CONSTRUCTION OF AN EXCAVATION This tutorial illustrates the use of PLAXIS for the analysis of submerged construction of an excavation. Most of the program features that were used in Tutorial
More informationStudy of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket
RESEARCH ARTICLE OPEN ACCESS Study of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket Gowtham K L*, Shivashankar R. Srivatsa** *(Department of Mechanical Engineering, B. M.
More informationMODELING AND ANALYSIS OF LATTICE TOWERS WITH MORE ACCURATE MODELS
Advanced Steel Construction Vol. 3, No. 2, pp. 565-582 (2007) 565 MODELING AND ANALYSIS OF LATTICE TOWERS WITH MORE ACCURATE MODELS Wenjiang Kang 1, F. Albermani 2, S. Kitipornchai 1 and Heung-Fai Lam
More informationANALYSIS OF BOX CULVERT - COST OPTIMIZATION FOR DIFFERENT ASPECT RATIOS OF CELL
ANALYSIS OF BOX CULVERT - COST OPTIMIZATION FOR DIFFERENT ASPECT RATIOS OF CELL M.G. Kalyanshetti 1, S.A. Gosavi 2 1 Assistant professor, Civil Engineering Department, Walchand Institute of Technology,
More informationSEMI-RIGID JOINTS TO TUBULAR COLUMNS AND THEIR USE IN SEMI-CONTINUOUS FRAME DESIGN
SEMI-RIGID JOINTS TO TUBULAR COLUMNS AND THEIR USE IN SEMI-CONTINUOUS FRAME DESIGN A thesis submitted to the University of Manchester for the degree of Doctor of Philosophy in the Faculty of Engineering
More informationNumerical Analysis of Buried Steel Pipelines
Numerical Analysis of Buried Steel Pipelines Charis J. Gantes1, Vasileios Melissianos1 1 School of Civil Engineering, Institute of Steel Structures, National Technical University of Athens, Greece ABSTRACT
More informationUsing MSC.Nastran for Explicit FEM Simulations
3. LS-DYNA Anwenderforum, Bamberg 2004 CAE / IT III Using MSC.Nastran for Explicit FEM Simulations Patrick Doelfs, Dr. Ingo Neubauer MSC.Software GmbH, D-81829 München, Patrick.Doelfs@mscsoftware.com Abstract:
More informationTutorial 1: Welded Frame - Problem Description
Tutorial 1: Welded Frame - Problem Description Introduction In this first tutorial, we will analyse a simple frame: firstly as a welded frame, and secondly as a pin jointed truss. In each case, we will
More informationBest Practices for Contact Modeling using ANSYS
Best Practices for Contact Modeling using ANSYS 朱永谊 / R&D Fellow ANSYS 1 2016 ANSYS, Inc. August 12, 2016 ANSYS UGM 2016 Why are these best practices important? Contact is the most common source of nonlinearity
More informationThe Effect of Element Formulation on the Prediction of Boost Effects in Numerical Tube Bending
The Effect of Element Formulation on the Prediction of Boost Effects in Numerical Tube Bending A. Bardelcik, M.J. Worswick Department of Mechanical Engineering, University of Waterloo, 200 University Ave.W.,
More informationChallenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure
Challenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure In the final year of his engineering degree course a student was introduced to finite element analysis and conducted an assessment
More informationIdentification of strain-rate sensitivity parameters of steel sheet by genetic algorithm optimisation
High Performance Structures and Materials III Identification of strain-rate sensitivity parameters of steel sheet by genetic algorithm optimisation G. Belingardi, G. Chiandussi & A. Ibba Dipartimento di
More informationANSYS Workbench Guide
ANSYS Workbench Guide Introduction This document serves as a step-by-step guide for conducting a Finite Element Analysis (FEA) using ANSYS Workbench. It will cover the use of the simulation package through
More informationTHE EFFECT OF THE FREE SURFACE ON THE SINGULAR STRESS FIELD AT THE FATIGUE CRACK FRONT
Journal of MECHANICAL ENGINEERING Strojnícky časopis, VOL 67 (2017), NO 2, 69-76 THE EFFECT OF THE FREE SURFACE ON THE SINGULAR STRESS FIELD AT THE FATIGUE CRACK FRONT OPLT Tomáš 1,2, POKORNÝ Pavel 2,
More informationLearning Module 8 Shape Optimization
Learning Module 8 Shape Optimization What is a Learning Module? Title Page Guide A Learning Module (LM) is a structured, concise, and self-sufficient learning resource. An LM provides the learner with
More information